Configurations in SOLIDWORKS parts and assemblies give you the ability to vary dimensions and control the suppression states of various features without needing to create a new document. This allows you to have multiple variations of one project within one file.
An example I often bring up is a washer; a washer is a simple component which comes in numerous sizes but the features used to create it will typically be the same. You can certainly have an individual part file for each size of washer or you can have one part file called “washer” which uses configurations to include all sizes. You can then choose which configuration you want to use as it is inserted into an assembly.
This can be very useful, but depending on how many configurations are in use, managing them can become difficult. So instead of manually activating each configuration and then adjusting their details you can implement SOLIDWORKS Design Tables, which will tabulate all relevant information into an easy to use Excel spreadsheet.
To help prepare yourself for using a Design Table in SOLIDWORKS, I often recommend naming features and dimensions so they are easy to recognize from a distance.Features can be renamed by slow double clicking on them in the FeatureTree, or select the feature and press F2 on your keyboard.
Sketch dimensions can be renamed via their Modify dialogue.
To create a Design Table you will go to Insert > Tables > Design Table. Here you may create a blank table, auto-create a table based on dimensions and features which already vary per configuration, or link the Design Table to an external Excel spreadsheet file. We will come back to this last option later.
In my example, I will be choosing the “Blank” option so I can pick and choose which items I would like to import into the table. I will then select which configurations, dimensions, features, and properties I would like to populate into the table.
Now that my table has been generated I can add additional configurations by filling in the row and relevant cells.
Next, I will left click in the graphics window, the table closes automatically, and the new configuration is created for me.
Now that the table has been created I can locate and modify it under the Tables folder on the Configurations tab.
Back in the table, I want to control the suppression state of the engraved text. I can add this feature as a column by simply double clicking it in the FeatureTree. You can also add dimensions as columns by double clicking them while they are visible.
From here I will fill in the cells in this column as needed. You can use the text [Unsuppress, U, 1] or [Suppress, S, 0] to control the suppression state of features in the table.
Linking to an External Excel Spreadsheet
Now that your table has been created you have the ability to export it as an external Excel spreadsheet and then link it back to the part. This gives users the ability to modify the Excel spreadsheet outside of SOLIDWORKS, adding their own rows for new configurations, and the next time SOLIDWORKS is opened it will update the part appropriately. Here are the steps to follow:
- Right click on the Design Table within the Tables folder on the Configuration tab.
- Select Save Table and save it as an Excel spreadsheet to your desired location.
- Right click again on the Design Table and choose the option Edit Feature.
- Select From File and browse for the spreadsheet. Also ensure you have Link to File selected.
That’s it! The best part about this tool, with the Link to File option selected there will be a back-and-forth communication between the SOLIDWORKS model and the spreadsheet. If you change the configurations in SOLIDWORKS it will update this external spreadsheet and if the spreadsheet is changed outside of SOLIDWORKS it will update the model the next time it is opened.
I hope you found this to be helpful! If you have any additional questions on Design Tables in SOLIDWORKS don’t hesitate to reach out to our support team or leave me a comment below. Plus, be sure to for future blogs discussing more advanced functions within SOLIDWORKS.
Written by Jesse Butwinick
Jesse Butwinick is an Application Engineer at Alignex, Inc. When Jesse isn’t teaching SOLIDWORKS classes or solving a customer’s biggest design frustration, he enjoys building furniture with SOLIDWORKS’ weldments design function and teaching himself how to use new technologies.